Engineering & PLMFree referencePDF, Excel, Word export

GD&T Characteristic, Datum and Tolerance Zone Reference

This table answers the questions that come up on every drawing review: does this control need a datum, what shape is the zone, and can I use MMC? It covers the 14 characteristics in the ASME Y14.5 family plus the common modifiers and the first two rules.

Download:
Characteristic or symbolGroupDatum referenceTolerance zoneMaterial condition modifiersPractical note
Straightness
Form
Never
Two parallel lines (surface line elements) or a cylinder (derived median line, diameter symbol)
MMC or LMC only when applied to a feature of size axis
Controls a line element or axis, not the whole surface. Surface straightness is checked per line element.
Flatness
Form
Never
Two parallel planes
MMC or LMC only when applied to the derived median plane of a feature of size
Must be smaller than any size tolerance on the same surface to be meaningful.
Circularity (roundness)
Form
Never
Two concentric circles in each cross-section
None
Evaluated one cross-section at a time, so a tapered part can be perfectly round at each section.
Cylindricity
Form
Never
Two coaxial cylinders
None
Combines circularity, straightness and taper in one control. Costly to inspect, use sparingly.
Profile of a line
Profile
Optional
Uniform boundary around the true profile of a cross-section, equally disposed unless noted
None normally
Used for 2D cross-sections such as airfoil sections, where each section is controlled separately.
Profile of a surface
Profile
Optional
Uniform 3D boundary around the true profile, equally disposed unless noted
None normally
With no datum it controls form only. With datums it controls location, orientation and form together.
Angularity
Orientation
Always
Two parallel planes at the basic angle, or a cylinder for an axis
MMC or LMC for a feature of size
Basic angle must be on the drawing, a plus/minus angle tolerance is a different control.
Perpendicularity
Orientation
Always
Two parallel planes 90 degrees to the datum, or a cylinder for an axis
MMC or LMC for a feature of size
Often the right control for a hole axis to a mounting face.
Parallelism
Orientation
Always
Two parallel planes parallel to the datum, or a cylinder for an axis
MMC or LMC for a feature of size
Surface parallelism also limits flatness of the surface to the same value.
Position
Location
Normally yes
Cylinder (diameter symbol), two parallel planes, or other boundary around the true position
MMC, LMC or RFS (RFS is the default)
Replaces coordinate plus/minus tolerancing for most holes and pins. Bonus tolerance applies under MMC or LMC.
Concentricity
Location
Always
Cylinder around the datum axis for derived median points
RFS only
Removed from ASME Y14.5-2018. Still seen on legacy drawings, use position or runout today.
Symmetry
Location
Always
Two parallel planes about the datum center plane for derived median points
RFS only
Removed from ASME Y14.5-2018. Use position or profile instead.
Circular runout
Runout
Always (axis)
Two concentric circles in each circular element, measured with a full indicator movement
RFS only
Checked per cross-section while rotating the part 360 degrees about the datum axis.
Total runout
Runout
Always (axis)
Two coaxial cylinders for a surface, or two planes for a face, over the whole surface
RFS only
Controls circularity, straightness, taper and wobble together. The indicator travels along the surface.
Maximum Material Condition (MMC)
Modifier
Not applicable
Not applicable
Applies to a feature of size and datum features of size
Smallest hole or largest pin. Gives bonus tolerance as the size departs from MMC.
Least Material Condition (LMC)
Modifier
Not applicable
Not applicable
Applies to a feature of size and datum features of size
Largest hole or smallest pin. Used for minimum wall thickness and edge distance.
Regardless of Feature Size (RFS)
Modifier
Not applicable
Not applicable
Default under Y14.5-2018 Rule 2 where no modifier is shown
The tolerance is fixed. The old circle S symbol was dropped in 2009.
Projected tolerance zone (P)
Modifier
Not applicable
Zone extends above the part surface by the stated height
Used with position or orientation of a threaded or press-fit hole
Controls the fastener location where it mates, not the hole in the part.
Free state (F)
Modifier
Not applicable
Not applicable
Nonrigid parts
Tolerance applies before restraint, used for thin or flexible parts.
Tangent plane (T)
Modifier
Not applicable
Plane contacting the high points of the surface
Orientation and flatness controls
Controls the plane of the surface contacts, ignoring form variation of the surface.
Statistical tolerance (ST)
Modifier
Not applicable
Not applicable
Requires statistical process control
Allows a wider tolerance when process control is demonstrated. Rare outside controlled programs.
Continuous feature (CF)
Modifier
Not applicable
Not applicable
Several features treated as one
Treats multiple surfaces or features as a single feature for the control.
Independency (I)
Modifier
Not applicable
Not applicable
Cancels the Rule 1 envelope requirement on a feature of size
Form is then controlled only by the geometric tolerance, not the size limits.
Rule 1 (envelope principle)
Rule
Not applicable
Perfect-form boundary at MMC
Individual features of size
Where size limits are shown, form cannot violate perfect form at MMC. Reduces the need for separate form callouts.
Rule 2 (RFS default)
Rule
Not applicable
Not applicable
All geometric tolerances
Under Y14.5-2018 RFS applies to the tolerance and datum features unless a modifier states otherwise.

Summary of ASME Y14.5 concepts for quick lookup. It is a study aid, not a substitute for the standard, which defines exact requirements and exceptions. Check which edition (2009 or 2018) the drawing cites, since concentricity and symmetry were removed in 2018 and some modifier rules changed. A tolerance zone listed as a cylinder applies when the diameter symbol is in the feature control frame.

Turn drawing callouts into inspection plans faster

Optional: we can discuss how a private assistant could read your drawing characteristics and propose an inspection method and gauge list.

Optional. The tool and every export work without this. No spam.

How to use the reference

Search for the characteristic or filter by group. The datum column tells you at a glance whether the control must reference datum features: form controls never do, orientation and runout always do, position almost always does, and profile may or may not. The zone column describes the shape of the tolerance zone the measured feature has to fit inside, which drives the inspection method. The modifier column states whether MMC or LMC can apply, which tells you if bonus tolerance is available and whether a functional gauge is an option.

  • Form controls: straightness, flatness, circularity, cylindricity.
  • Orientation controls: angularity, perpendicularity, parallelism.
  • Location: position, concentricity, symmetry (the last two removed in 2018).
  • Runout: circular and total, always RFS, measured from a datum axis.

Zones drive inspection

A cylindrical zone from a diameter symbol allows the axis to wander in any radial direction, which suits holes and pins. A pair of parallel planes limits a single direction, which suits slots and flat surfaces. A profile zone is a 3D boundary that can be checked with a CMM scan or a template. Understanding the zone also helps estimators: a total runout or cylindricity callout often means a dedicated setup and a slower inspection cycle than a simple size tolerance, which should show up in the quote.

Modifiers and bonus tolerance

MMC and LMC apply only to features of size, such as holes, pins, slots and tabs. Under MMC the tolerance grows as the feature moves away from its maximum material size, so a hole produced near its large limit has more position room, matching how a pin would still fit. LMC works the opposite way and is used to protect minimum wall or edge breakout. RFS leaves the tolerance fixed. Form, runout and surface-based controls generally do not take MMC or LMC, except for axis or median plane controls on a feature of size.

Edition differences

ASME Y14.5-2018 removed concentricity and symmetry, replaced them in practice with position, profile or runout, and clarified default RFS handling, so the old circle S symbol is not used. ISO GPS (ISO 1101) has a different set of rules, including a default independence principle rather than the envelope rule, so a drawing prepared to ISO needs different interpretation. When you receive a build-to-print package, confirm the standard and edition in the title block before reviewing callouts.

Frequently Asked Questions

Which GD&T controls do not need a datum?

The four form controls, straightness, flatness, circularity and cylindricity, never use datums because they only describe the shape of the feature itself. Profile of a line or surface can be used with or without datums. Orientation, location and runout generally require them.

Can I use MMC on a flatness callout?

Only when flatness is applied to the derived median plane of a feature of size, such as the center plane of a slot. When applied to a surface, flatness takes no material condition modifier, because a surface has no size to depart from.

What happened to concentricity and symmetry?

They were removed from ASME Y14.5 in the 2018 revision because they are difficult to measure and rarely express the real functional requirement. Designers now use position, profile or runout instead. They may still appear on older drawings, so a quoting team needs to recognize them.

What is the difference between runout and position?

Runout is measured by rotating the part about a datum axis with an indicator and controls surface variation relative to that axis, always at RFS. Position controls the location of a feature's axis or center within a zone and can use MMC for bonus tolerance.

If your shop interprets callouts into inspection plans by hand, Netray can help build a private agent that reads drawing characteristics and drafts the plan and gauge list for your engineers to approve.

Talk to an ExpertExplore More Free Tools

Related Tools

Engineering & PLM

GD&T Symbols Reference Table

A searchable list of the 14 GD&T geometric characteristics and common modifiers with category, datum use and tolerance zone shape.

Engineering & PLM

Datum Reference Frame Definition Template

A one-page record of how datums A, B and C are established, which degrees of freedom they constrain and how the fixture and CMM should locate the part.

Quality & Inspection

True Position CMM Results Evaluation Worksheet

Evaluate a whole feature pattern at once: convert CMM X/Y deviations to diametral true position, add MMC bonus, and see pass/fail, percent of tolerance used and margin per hole.

Engineering & PLM

Bonus Tolerance (MMC) Position Calculator

Calculates the bonus tolerance gained as a feature departs from maximum material condition and compares the total allowed position zone to the measured error.

Engineering & PLM

Fixed and Floating Fastener Position Tolerance Calculator

Calculate the position tolerance for clearance holes using the floating and fixed fastener formulas, split it between parts and check the hole at LMC.

More Engineering & PLM tools

See all
Back to All Tools

Keep exploring

Free tools